CNC Router - Techno LC 59120

From Tech Valley Center of Gravity Wiki
Jump to navigation Jump to search


A CNC router for cutting, engraving, and shaping sheet woods, plastics, and foams.

The machine and the work area have been set up to be accommodating to those who are new to CNC machining. Tooling is available with pre-determined feed and speed rates for typical materials. One-on-one classes are available for users of all skill levels. All users must at the very least take an Operational Checkout class to ensure they have sufficient knowledge to run the machine without damaging it or themselves.


Axis: 3

Material Width: 59"

Material Length: 120"

Gantry Clearance: 5"

Z Travel: 8.9"

Power: 5 HP

Spindle Speed: 6,000 - 18,000 RPM (100 - 300 Hz)

  • Spindle speed can only be manually controlled on the machine. There is no communication between the G-Code specified speed and the spindle (speed is constant for the length of the file)

Feed Rate: 240 IPM

Safety Rules

  • Risk of eye damage. Wear eye protection.
  • Risk of hearing damage. Wear hearing protection when machine is in use.
  • Risk of pinching, crushing, and entanglement.
    • Keep body parts away from machine when in use.
    • Secure loose clothing, jewelry, hair.
    • Press Emergency Stop button during tooling changes.
  • Risk of fire.
    • Follow material manufacturer’s recommended cutting speeds.
    • Do not use dull tooling.
  • Risk of cuts. Wear gloves when handling material and cutting tools.


  • Dust collector shall be on, EXCEPT when cutting metals.
  • Do not leave machine unattended.
  • Ensure collet is flush with nut after torqueing.
  • Vacuum is insufficient for material smaller than 1 square foot. Affix material to waste board with either composite nails, double-sided tape, or t-slot clamps.  
  • Compressed air for nail gun use only. Do not blow off table. Use vacuum for sawdust.
  • Router is not capable of cutting solid metals (no coolant, insufficient torque). Aluminum and steel clad panels are acceptable (aluminum composite panel and steel composite panel).
  • Only use CoG supplied tooling within recommended feed rate ranges. To use other tooling, submit a link to the manufacturer's description and recommended feed/speed rates to


NOTE: These materials are not a substitute for hands-on training with an experienced user.



  • Spindle Speed is manually controlled by the knob on the VFD, and is displayed in Hertz. Gcode specified speeds are ignored.
  • Feed Rates are manually entered into the software interface.
    • The Techno software does not understand the post-processor's feed rates. Feedrate will remain a constant throughout the operation. If different feed rates are necessary, your gcode will need to be broken up into segments, with each segment having a consistent feed rate.
  • Set your X, Y and Z zero before running a new program. Loading a new file may reset your origin point.
  • Before starting a program, the machine will move to Z0. If your origin is on the table, the tool will penetrate through your material. This is a "feature" of the software on this controller, corrected on subsequent controllers.

Fusion360 CAM

Fusion360 is the CAM software used for this machine and all associated training. While it is possible to make use of other software, nothing else has been tried yet. While the CoG is open to allowing different CAM software, keep in mind there will be some trial and error in figuring out post-processor files and correct formatting settings. It is also possible to import your CAD model from another software into Fusion for CAM work, but things tend to go easier if CAD and CAM are done in the same environment.

Techno Post-Processor

  • Download the most recent Techno CNC post-processor from the Autodesk Website. Search for "Techno CNC"
  • The machine will start the program from wherever its current position is. The post-processor directs movement in X and Y before the Z, which will result in either a crash (if Z is set below material top) or the tool dragging across the material (if Z is set at the material top). Review the opening movements in your gcode, and ensure that the tool's starting location will not cause unwanted problems.
  • The Techno post-processor provided by Autodesk isn't fully compatible with our machine, due to the age of our machine's software. The software doesn't recognize all of Fusion's capabilities, and will return errors or incorrect path geometries when it comes across g-code segments it doesn't understand. The most common error is giant arcs inserted into the toolpath. The errors can be avoided by using the settings below. If you find any more errors or solutions, please document them here.

All Operations

  • Uncheck Lead-In (Entry) or Lead-Out (Exit).
  • Ramp Type: Use any ramp type other than Helix.
  • Occasionally, the giant arcs can be prevented by setting the Machining Boundary to "Bounding box" with "Additional Offset" set to 1 inch.


  • Set direction to climb or conventional milling only. "Both Ways" doesn't work.

2D Pocket

  • Passes: Don't select Both Ways. Causes errors at the bottom of the pocket.

Post Process Settings (different than default):

  • Allow Helical Moves: No
  • (Built-in) High feedrate mapping: Preserve single axis rapid movement
  • (Built-in) Maximum circular radius: 10
  • Force IJK: No
  • Machine type: HD Series
  • Use tool changer: No
  • Write machine: No

Operation Instructions

See CNC Router - Techno LC 59120 Instructions


Overview of Fusion360 CAM: